Jump to navigation Jump to search

Shop Area: Woodshop

Tool: CNC Router

Requires in-person training: Yes 

Procedure Number

UG 110-08, Rev. 1





We have three CNC routers:

  • Shapeoko 2 – CNC, a small, light duty but simple to use machine with a 2x2' cutting area.
  • Phoenix - a 4x4', heavy duty machine running LinuxCNC
  • AXYZ 4008 - a 4x8', heavy duty machine running LinuxCNC

Shapeoko 2 – CNC Router.png


  • Safety glasses to be worn when making a cut.
  • Ear protection recommended.
  • Before operating, remove tie, rings, watches and other jewelry, and roll sleeves up past the elbows. Remove all loose clothing and confine long hair.
  • Non-slip footwear or anti-skid floor strips are recommended.
  • Do not wear gloves.
  • Do not leave workstation until cut is complete.



General Controls and Configuration

The Phoenix and AXYZ CNC routers can both be controlled using their respective gamepad controllers. The button configuration is shown below.

Controller movelist.png


There are many ways to complete this workflow, but included in this section are descriptions of how to make a successful cut with two different sets of software. The first is the most simple, the second more challenging but more powerful.

Inkscape -> SheetCAM -> LinuxCNC

One method of getting from idea to CNC routed part is to create your CAD design in Inkscape, then use SheetCAM to generate the tool paths. If carving a 2D design like a sign, this is the quickest and simplest method. Below is the general outline of this approach.

  1. Import drawing into SheetCAM (svg or dxf)
  2. Check machine options (Options -> Machine)
    1. Postprocessor -> LinuxCNC
    2. Postprocessor -> output units
  3. Set job options (Options -> Job Options)
    1. Set material dimensions
    2. Set origin
  4. Assign contours to layers
  5. Create tools to be used
  6. Create operations that assign tools to layers
    1. Set feeds and speeds (flip to other side for help)
  7. Visualize the job with Mode -> Simulation
  8. Create gcode: File -> Run Post Processor
  9. Transfer gcode file to cncrouter computer using USB stick or /vsfs01/share directory
  10. Open gcode file from LinuxCNC
  11. Insert tool in CNC router
  12. Clamp down workpiece (Always use a spoil board!)
  13. Turn on CNC router by rotating E-stop button clockwise
  14. Home machine by clicking Home All in LinuxCNC or by pressing Start + Select at the same time
  15. Move tool to origin and set the x, y, and z coordinates to zero by click Touch Off in LinuxCNC or by pressing Select + Direction Pad
  16. Confirm that tool won’t collide with hold-downs by manually jogging machine around the path
  17. Turn on dust collector
  18. Run operation
  19. Turn off dust collector and tidy up

FreeCAD -> LinuxCNC

Another method of using the CNC router is to use a program like FreeCAD to generate your 2D or 3D model, then also doing the CAM within FreeCAD. The benefit to this approach is that everything is done in a single program, and that the program is significantly more powerful and capable of handling 3D designs.

Easel to Shapeoko

The Shapeoko can also be controlled with the workflow described above, but it also comes with a software package called Easel, which is meant to simplify the process.

  1. Login to Easel using the credentials found on the CNC router.
  2. Draw a simple design directly in Easel, or design something in Inkscape, save as an SVG and import into Easel.
  3. In the top right of the Easel interface, choose your material type (this determines safe feed rates) and material dimensions
  4. Select the bit size you intend to use
  5. Arrange your design in the workspace and set the final depth of cut that you'd like.
  6. Unplug the Shapeoko
  7. Manually move the router head to the front left corner, and manually rotate the Z-screw until the tip of the router bit is touching the top of your workpiece. This is your zero position that corresponds to the bottom left corner of your Easel workspace.
  8. Plug in the Shapeoko
  9. Click the Carve button in the very top right to start cutting the design.
  10. Remain nearby until the cut is finished


== General Issues ==  Turn the machine on, so that the motors energize, but don't tell it to move. Do not turn the spindle on. Try to wiggle the spindle left and right by hand. Can you move it? If you can, watch carefully to see what moves with it. Does the belt move but the pulley doesn't turn? You have a loose belt. Does the pulley turn too? You have a loose pulley set screw. Does the entire gantry move with respect to the stationary rails? You have loose V-wheels or eccentric spacers. And so on. Repeat for back and forth movement, and up and down too, if that's also causing problems.

Machine won't start

The console window will show the command being sent and a confirmation of "ok". However, the active state goes to "Queue" and never returns to "Idle.

  • Auto cycle start has been turned off - Note that turning off auto cycle start requires that one begin the machine manually.
  • Previous operation was quit from the Communication / Control program w/o disconnecting. Restart the computer system.
  • USB port has gone into low-power mode.  Energy-savings features can interfere w/ sending data to the Arduino. Do not let the controlling machine go into low power mode,
  • Corrupt Grbl settings.  It is possible for a power interruption or other issue to result in invalid data being stored, making it impossible for Grbl, which has minimal error checking, to process any commands.

Machine jogs, but won't respond to downloaded file

The machine will respond to single commands, but will not accept a downloaded file and will endlessly repeat some statement to the console.

  • Grbl software installation corrupt. Reflash Grbl.
  • Corrupt Grbl settings.  It is possible for a power interruption or other issue to result in invalid data being stored, making it impossible for Grbl, which has minimal error checking, to process any commands.

Machine won't hold position

Set Grbl setting for "step idle delay" in milliseconds to 255 (suggested default). It will always energize the motors to a hold position. If set to some other value, motors will be turned off after the specified time.

Toolpath Differs from Expected

If the machine's behavior doesn't match what is simulated.

  • software bug - Grbl is very reliable, so unlikely to be in the firmware.
    • Carbide Motion 4 ought to give an error message on any G-Code which it can't properly send on to the machine, and Carbide Create ought not make any code which doesn't work properly
  • file problem - an example of this would be setting safety / retract height too high, using the wrong post-processor, or enabling a feature such as XY datum in Vectric Vcarve.
  • machine misconfiguration / user error - this can be a lot of things, occasionally overlapping with the above, for example setting safety / retract height and the Z-axis zero so that when the machine lifts to safety height it bumps against and loses steps against the top stop, so that the Z-axis height isn't correct.
  • mechanical machine setup - these ought to be covered by the machine Operating Checklist --- frequent things to check:
    • Check pulley set screws
    • Check V wheels / eccentric nuts
    • Belt tension, the Z-axis belt in particular needs to be guitar string tight (but careful not to bend the motor shaft).
    • Electronics - it's possible for a wire or connector to break or for a lost connection or excessive current generated by the stepper motors or a stray static spark to damage the stepper driver or controller.

Radius of corners is different

Stairstepped diagonals, jagged circles/curves, loud squealing or 'ker-chunka' thuds, gantry chattering, mis-aligned edges.  A useful troubleshooting technique for this is to listen to the machine:

  • If it sounds awful = loose wire (or the stepper driver going into thermal shutdown).
  • If it sounds normal = loose set screw (or other mechanical issue such as loose belts).

File worked previously, doesn't work now

Reaching limits of machine.

  • Either overheating or reaching acceleration limits.
  • Steppers may be entering thermal shutdown, add active cooling.
  • Machine is operating at the limits of its acceleration. Slow down feed speeds and max acceleration in GRBL.
  • Endmill no longer sharp, spindle not working properly (rotating in wrong direction). If the machine is not able to properly cut, then it will not be able to move along the desired path, since it will not be clear.
  • A spindle which is not working properly may put out EMI which will interfere w/ the movement of the stepper motors. Brushes on a router are a consumable part and must be replaced periodically.

Steppers are missing steps

  • Drivers overheating - Position the fan so that in blows across both the top and bottom of the drivers. Airflow does the most, followed by a heatsink on top of the chip. Note that this may also be caused by setting the current too high.
  • Steppers being run too fast - GRBL has a maximum speed that it can drive stepper motors at. Because the X and Y axis are belt driven while the Z is threaded rod drive, it is very easy to set the x/y Default Feed speed faster than the Z axis can be signaled. Cut your default feed and test.
  • Feed rate too fast - The harder the material being cut, the more torque the steppers have to resist. If you're feeding too fast, this can overcome the holding torque of your motors.
  • Axis binding - Check that all of your v-wheels rotate freely when bolted and tightened, as some of the tolerance problems in the v-wheel components can be bad enough to cause the bearings to bind and the v-wheel to be stiff. If you're not using a drive shaft or dual Y axis steppers and your v-wheels or rails are adjusted incorrectly, the Y axis can bind and overwhelm the rated torque on your steppers. Also check that you've tensioned the eccentric spacers correctly. The v-wheels should be firmly planted but should not be so tight that there is any deflection/bowing in the plate, and should be easy to slide along the rails.
  • Axis stalling - If you're using a drive shaft it is possible to have one pulley slip while the other will continue to drive the machine. Any instance of slippage should be investigated by checking the set screws on the pulleys.
  • Electrical brownout - The power supply does draw a fair bit of power for the stepper motors, minimize other power drawing sources.
  • Electrical interference - The spindle and motors put out quite a bit of electrical interference. This may cause random or irregular deviations in the movement of the machine. Shield the wires.
  • Loose Idler - Odd distortions, all tending towards a particular direction may be caused by an idler pulley being loose.

Deviations in slots when cutting

The bit is pulled along creating random path deviations which get worse as one gets deeper into a slot.

  • Spindle is more powerful than the machine can manage.  Spindle not kept up with the balance of the machine, the machine flexing along the Z-axis may flex and allow the bit to rub up against the edge of a slot where the cutting action will then pull the machine further along. Make the X-axis more rigid.

Deviations in shapes when cutting

The machine lags behind at changes of direction, distorting shapes and creating flat edge at the extrema of rounded forms.

  • Backlash/Insufficient belt tension - If your belts are too lose, the machine will shift w/ the cutting forces, distorting shapes. Machines w/ threaded rod will have similar difficulties if nuts do not have anti-backlash features.

Z-axis cuts more deeply than expected

The bit is pulled along going deeper into the material than it should.

  • Acceleration / movement too fast.  The Z-axis is limited in its acceleration and top speed by the torque of the motor. If it is able to move down okay, but will not move up reliably, then the acceleration or movement may be too fast or high. Some G-code senders have an option to limit the Z-axis speed.
  • Spindle is loose in its mounts, Z-axis plunge rate too fast causing the machine to go deeper. Always check to ensure the spindle is secure. Always be cautious with Z-axis plunge rates, especially when using CAM tools which lack spiral or ramp Z-axis moves.
  • Z-axis motor is over-heating, causing the machine to fail to move up on negative moves (it's more difficult to lift the spindle than to lower it) causing it to cumulatively go deeper. Adjust the current, consider adding heat sinks and/or a fan to cool the stepper drivers.
  • End mill loose in collet --- this can also cause other path deviations as the needed cutting forces are increased beyond the machine's capabilities. Tighten collet.

Z-axis cuts at odd angles when cutting thin stock

The bit is pulling the material up or twisting it as it cuts.

  • Switch to a down-cutting spiral bit --- check and ensure the bit is sharp.
  • Lines are not straight, circles not round, dog bone pattern at corners, cut quality poor - DC spindle wired to run backwards.
    • A damaged or dull end mill.
    • Milling direction may be wrong.
  • Repeating curve/wobble - Bad bearing or V-wheel

Material Stock Melting or Burning

Smoke, fire, material build-up on tooling, poor cut edges (plastic) or burn marks (wood).

  • RPM too high / Feed rate too low The surface of your tooling is moving too fast relative to the material. This leads to 'dwell', where the tooling rubs against the material to create a significant amount of heat.
    • Increase your feed rate (higher mm/minute). Increasing your feed rate decreases the speed difference between the edge of your tooling and the material, reducing friction. GRBL has some limitations on feed, especially in smaller parts and curves, so this is not always possible.
    • Slow your spindle (lower RPM). If your router or dremel has variable speeds, turn it down. This, however, usually reduces the available torque, which can in turn lead to stalling your spindle during the cut.

Persistent Ridges

Endmill is either bent or deflecting.

Bit Chatter

Loud chattering, jagged cut edges, snapped tooling. Feed rates too high or loose frame.

  • Slow the feed - If your tooling is trying to bite too much material, it will be under much higher stresses, pushing away or into the material much more than usual. Slowing down your feed rate can reduce this.
  • Tighten the frame - Especially if you did not use loctite when assembling, bolts can work loose over time (or never having been tightened sufficiently), greatly reducing the rigidity of the frame - this rigidity is what a CNC uses to move the tool where it is supposed to be. Tightening everything up will help this.
  • Another possibility is the spindle carriage plate is running off the bottom of the rail, esp. w/ the new style plate.

Machine Chatters/Vibrates

Chattering, buzzing.  Tighten wheels.


                                END OF THE PROCEDURE